- We will now use the "Revolve Boss Base" command
to revolve the front shaft of our flywheel.
The reason for using this tool instead of the
"Extrude Boss Base" is so we can capture our
required profile from a single sketch and extrude.
Start a new sketch on the right plane.
Using the "Spacebar" key to bring up the
in-context "Do Your Orientations" dialog,
we have easy access to the "Normal to" icon,
which rotates the graphics view normal to our screen.
Note the shortcut key is "Control+8",
if you prefer to use that instead.
Select the icon for a normal-to orientation.
Follow my lead as I sketch the required profile,
select the line tool, starting on the midpoint
of the front edge of the underlying geometry.
Sketch a vertical line,
then a horizontal.
Add a couple of steps similar to this.
Add another horizontal line, then a vertical line
down 'til we are perpendicular with the origin,
which is denoted for us by the blue inference line
and then back to our start point.
Note that the reason I started on the front edge
of the existing extrude, and not on the origin,
is so the front shaft will maintain its length,
relevant to that first.
If the underlying extrusion depth had to change,
if we used the origin instead,
it would simply be fixed by that
and give us undesired results.
"Escape" to cancel the active command.
Make the first step's vertical
and horizontal lines equal to each other,
so we only need to apply one dimension.
Select the "Smart Dimension" tool,
set the right vertical line to 43 millimeters,
the top horizontal line to 64 millimeters,
step one to six millimeters,
step two to 12 millimeters,
and this horizontal line to 54 millimeters.
From the "Features" tab, select the
"Revolve Boss Base" command.
Note the "Axis of Revolution" box
is preselected in the command's properties,
since we need to specify an axis.
Whenever I am adjusting feature properties,
I prefer to change my graphics view to the
default tri-metric view, so I can properly see the result
of my extrusion for additional adjustments, if needed.
We will select the bottom horizontal line
in the graphics view as our axis of revolution.
Complete the command.
On the front face of the newly-created extrusion,
we will create another extrusion.
With the face selected in the graphics view,
from the context toolbar, select the "Sketch" icon.
With the face still selected,
select the "Convert Entities" command,
which automatically creates a circle
from the underlying geometry.
Now if the underlying geometry changes, so will the sketch.
Do an extrude.
Make the length 32 millimeters,
with a draft of eight degrees, and complete the command.
Note I activated the draft dialog by
selecting this "Draft" icon.
Let's do the back shaft while we are at it.
On the back face of our flywheel, start a new sketch.
And sketch a circle with its center point
vertical to the origin.
Create a vertical relation
from the center point to the origin,
so the circle is constrained in that position.
Make the circle equal to the top arc.
Dimension the circle 60 millimeters from the origin.
Extrude the circle 50 millimeters,
and your model should now look like this.
We'll leave it at that and I'll see you in the next video.